# SOLIDWORKS Reverse Engineering - Modélisation des surfaces et problème des pièces héritées - Partie 1

Article by Mike Walloch, CSWE updated January 2, 2023

###### Article

Reverse Engineering is a problem many companies face. TriMech offers powerful tools, such as 3D scanners, to make the job a breeze for those who deal with it regularly. But what about those who occasionally need to re-create something for which the original documentation is missing or incomplete? We will look at how surface modeling in SOLIDWORKS can help solve these problems.

Bouton strié - Pièce finie

The part shown above looks simple at first glance. The original is a molded plastic part. The drawing is manual and shows a pattern of 90 ridges around the outside of the knob. Unfortunately, it only gives us overall dimensions for the part, and essentially no information about the geometry of the individual ridges themselves. No angles, no radii, no depth for the grooves, etc. Not only that, but the ridges and grooves themselves bend inward in a transitional area and start tapering towards the central axis. Not so simple after all.

Original Part – Transition Area

Time to grab some calipers and start thinking outside of the box! Thanks to Brian Mitchell and Austin White at Barrett Plastics Inc. of Harrison, Arkansas for providing us with this modeling challenge.

## First Attempts

It seems obvious that the 90 ridges and grooves need to be broken down into one 4° slice, and then patterned to create the full 360° part. The profile could be a single ridge flanked by two halves of a groove, or a groove flanked by two halves of a ridge. The outside dimensions were easier to measure than the inside dimensions, so we used the centers of two ridges as the edges of the profile, and a groove as the center of it. In this image, the green lines mark the edges of the 4° profile slice.

Ridge and Groove Profiles

All our attempts to use standard solid modeling methods to re-create the ridges in the transition area after they start tapering in towards the central axis of the part failed. Our Sweep and Loft Features using 2D closed profiles and sketched guide curves did not blend smoothly after a Circular Pattern. Time to turn to surface modeling.

## Surface Modeling – Setup

We laid out a plan of attack by creating reference planes, a skeleton 3D sketch, and 2D path and profile sketches. We kept each sketch as simple as possible to avoid over-complicating the problem.

Mise en place initiale - Plans et croquis

The bottom of the part will be on the Top Plane. The ridges and grooves start on the Start Plane, and the tops of the ridges are coincident to the End Plane. A groove is the center of the pattern and lines up with the Right Plane (not shown). The Path Sketch (red) sits on the Guide Plane, which is rotated 2° from the Right Plane. The Skeleton sketch (magenta) is used as a point of reference for other sketches.

Path Sketch

The Path Sketch (black) was created using two lines and an arc on the Guide Plane. Then the Fit Spline command was used to convert them into a single spline to provide a smooth path for a Swept Surface.

Croquis de profil

The Profile Sketch (black) only has a line, an arc, and 6 relations in it. This is enough to create a Swept Surface defining half of a single ridge.

Creating the first Slice – Surface Modeling
The Swept Surface gives us the first ‘peak’ of a ridge and one of its sides. A Mirror gives us another peak and the beginning of a groove between them. Due to the tapering, the surfaces overlap and need to be trimmed using the Trim Surface feature. Then the groove can be formed with a Face Fillet.

Swept Surface

Miroir

Surface de la garniture

Face Fillet

## Path to a Solid Model – Surface Modeling in SOLIDWORKS

We must now choose how to use this surface body to create the final part. One approach would be to continue using surface modeling tools to create the entire exterior of the finished part, then convert it to a solid body. Another approach would be to use surface modeling tools to create a single, solid 4° slice of the finished part, then use solid modeling tools from there. Let’s look at the first approach and stick to surface modeling for most of the design.

Circular Pattern, Knit Surface, and Planar Surface

A Circular Pattern of the existing surface body results in 90 surface bodies forming a full circle. A Knit Surface feature joins them into a single body. A Planar Surface closes off the bottom. There are a lot of curved faces involved in these operations, and it takes a fair bit of time to process.

Extruded Surface and Trim Surface

Extruding a cylindrical surface from the Top Plane past the existing surface body gives us a trimming tool. Trim Surface features result in a nearly complete exterior of the part, with only the top and bottom left open.

Planar Surface, Knit Surface, and Thicken

Planar Surfaces can now be created to cap off the top and bottom, and the whole thing can be combined into a single air-tight surface body with Knit Surface. Finally, a Thicken feature converts the hollow surface body into a single solid body. Now we can add our finishing touches using standard solid modeling tools.

Touches de finition - Filets de coupe et de bordure extrudés

## Performance Concerns

I used SOLIDWORKS for nearly two decades before I took the Surface Modeling class. There is an old saying, “If you give a small boy a hammer, he’ll find that everything he encounters needs pounding.” Well, my newfound surfacing skills were like a hammer in the hands of a small boy there for a while. I suddenly saw uses for surface modeling in lots of places. Unfortunately, not all paths to get from problem to solution are created equal in terms of SOLIDWORKS performance. This problem required some surface modeling. But this approach resulted in a model that is almost all surfacing techniques until the very end. Performance Evaluation reports a total rebuild time of 31.45 seconds. This is far from ideal. In Part 2 we’ll look at a superior hybrid modeling approach.

SOLIDWORKS Reverse Engineering – Surface Modeling and the Legacy Part Problem – Part 2 continues here.

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### Mike Walloch, CSWE

Mike Walloch est un expert SOLIDWORKS certifié (CSWE) et travaille en tant que consultant en processus et en formation chez TriMech.